Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronic Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

Thermistor Hspice model

Status
Not open for further replies.

integ52002

Newbie level 6
Joined
Mar 25, 2009
Messages
12
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,373
Hi guys, I have been trying to design my temperature protection. I am using a thermistor. I would like to simulate it (temp sweep) in Hspice but I dont know how to model a thermsitor. Until I found this: http://www.hagtech.com/pdf/ntc.pdf
I got the spice netlist from here and it was successful. The R of thermistor varies exponentially. But i dont understand the syntax and I dont know how to model the particular thermistor by changing the parameters in the sample spice.
Is there anyone can give me advice about this please. ^^

ps. is there anyone can give me advice onn how to convert the data (R vs temp response) into an hspice model for simulation?
 
Last edited:

LvW

Advanced Member level 5
Joined
May 7, 2008
Messages
5,817
Helped
1,738
Reputation
3,478
Reaction score
1,337
Trophy points
1,393
Location
Germany
Activity points
39,029
May be the link doesn't work anymore.
Therefore, I'm going to send you a scanned copy of the original (pdf attachement).
The model is described in PSpice notation; however, i think there will be no problem to translate it to HSpice.
Any questions?
 

Attachments


FvM

Super Moderator
Staff member
Joined
Jan 22, 2008
Messages
47,440
Helped
14,034
Reputation
28,321
Reaction score
12,684
Trophy points
1,393
Location
Bochum, Germany
Activity points
275,931
In addition to the good solution by LvW, that's based on the ideal exponential thermistor characteristic, I try to answer the original question.

The first point is to understand the SPICE polynomial controlled source model, that's used for the quoted netlist. You should be able to find the explanation in SPICE textbooks and e.g. in the HSPICE Simulation and Analysis User Guide.

The second point is how to derive polynomial parameters from an empirical resistance versus temperature characteristic. The method is called curve fitting and can be easily performed with a spreadsheet calculator, e.g. MS Excel. Polynomial fit of a given order is an option in the Excel diagram window.
 

integ52002

Newbie level 6
Joined
Mar 25, 2009
Messages
12
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,373
Lvw and FvM thank you masters...

I am still trying to understand the other files u gave me and the explanations. But I would like to get back to my question again.
From http://www.hagtech.com/pdf/ntc.pdf we could see the table A showing the Resistance vs temperature. My question is how can I convert this table to the polynomial shown in the spice netlist. DO you have any idea how can I generate this polynomial so I could run the Thermistor model I need to simulate?
Please advice.

Thank you very much!!!
 

FvM

Super Moderator
Staff member
Joined
Jan 22, 2008
Messages
47,440
Helped
14,034
Reputation
28,321
Reaction score
12,684
Trophy points
1,393
Location
Bochum, Germany
Activity points
275,931
Yes, I already suggested a method. Enter the values in MS Excel, display an XY diagram, add a polynomial trendline and show it's parameters. MS EXCEL provides up to 6th order, which is sufficient in my opinion.
 

LvW

Advanced Member level 5
Joined
May 7, 2008
Messages
5,817
Helped
1,738
Reputation
3,478
Reaction score
1,337
Trophy points
1,393
Location
Germany
Activity points
39,029
Why not directly use a table as an input to describe the current-voltage relationship?
In PSpice there is a controlled source "Etable" that allows this procedure - and I suppose, HSpice will offer it also?
 

integ52002

Newbie level 6
Joined
Mar 25, 2009
Messages
12
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,373
FvM,

Hi Sir. I already generated the polynomial threadline (of 6th order) in Excel for Gout. But I want to know what are these Gout and Eout syntax here.
I know the Coeff's generated in Excel will be used in the Gout of the netlist. But what about Eout? How can I generate these Eout poly values? http://www.hagtech.com/pdf/ntc.pdf
Please advice.
Thank you very much for the advice!
 

FvM

Super Moderator
Staff member
Joined
Jan 22, 2008
Messages
47,440
Helped
14,034
Reputation
28,321
Reaction score
12,684
Trophy points
1,393
Location
Bochum, Germany
Activity points
275,931
The Eout in the simulation circuit hasn't to do with the thermistor characteristics. It's a multiplier, used to generate the resistor's C/V dependency. It's just one of many possible ways to play around with SPICE elements in a behavioral model. You can copy it or design your own way to simulate a resistor. I had thought, that a current controlled voltage source (H element) would be a more straightforward way to model a resistor.

P.S.:
Why not directly use a table as an input to describe the current-voltage relationship?
A table statement will implement a piecewise linear function, so you'll need much more sampling points for a smooth representation of an exponential characteristic. It's also not particularly suited for a polynomial fitting, by the way. So your previous suggestion to use an exponential function is basically the better way.
 
Last edited:

Status
Not open for further replies.
Toggle Sidebar

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top